I am having an issue when I open a drawing I have completed. When I open the drawing, the dimensions and notes are moved all over the place. I have tried to rebuild both the drawing and the part thinking it would move the dimensions and notes back but it doesn't work. It is very frustrating because I can't simply move the dimensions back to where I want them because they are referenced to an entirely different portion of the part. I have to pretty much start all over. I am using ordinate dimensions. Does anyone know why this is happening and how to prevent it from happening? I have Solidworks 2018.

Those are the little ONE and TWO things that would be nice if it's fixed... This is a random, kind of rare occurrence that has happened for years, it gets frustrating if and when I miss it and have all the drawings printed... I've tried to find a way to make it happen consistently, but could never figure it out, so by the time you notify the VAR, everything is ok and you can't get it to repeat again, until the next time which could be hours, days or months...

Well, it's premature to call this a bug, per se. It's actually a wide range of possibilities that may be workflow related. Configuration changes/major changes to geometry, system settings and document properties, shifting view positions (perhaps caused by changes to geometry, including hide/shown bodies), etc. Depending on how notes (leadered and unleadered) are attached to drawing views, this could even explain note placement changes too. If Adam is not aware what might be causing the shifts, he should review the document with his reseller to determine what's going on.

Premature since 1987 - this has happened for years, it didn't just show up. What is the definition of a Bug? Most "Bugs" are easy to reproduce, this doesn't act the same as a bug, more like a little glitch in the programming...

It is definitely as you mentioned in your reply, workflow could have a lot to do with it, shifting geometry etc... but it also has to do with "Drifting" views, especially if you have a parametric Assembly.

It's not the biggest glitch type of issue, just that little thorn that rips your arm once in a great while......

Depending on your scenario, there are one or several document and system settings that may apply to the behavior you are seeing. Try setting these:

System Options>Drawings>Reduce spacing when dimensions are deleted or edited (add or change tolerance, text etc..) - Uncheck This setting allows SOLIDWORKS to keep your dimensions offset to distances defined in your Document Properties. This is a live setting that will always apply changes to dimensions when SOLIDWORKS detects dimensions do not follow offset rules. This is the most likely culprit to the behavior you see.

Document Properties>Dimensions>Annotation view layout - Uncheck This setting applies your placement of dimensions in the model to your drawing. This is a very unlikely culprit to the behavior you see, unless you are making extensive use of model items.

Document Properties>Dimensions>Center between extension lines - Uncheck This setting allows SOLIDWORKS to make sure your dimension text for linear dimensions is always centered between the extension lines. This is a possible culprit for the behavior you see.

These are the automated dimension trinity of settings that you turn off when you want to fully control of dimension placement instead of entrusting SOLIDWORKS to help you. These settings are for some people, but obviously not all.

Edit: HOWEVER, these settings do not apply to Notes. Nor do these settings cause dimensions to move to wild locations on the drawings (quite the opposite, actually). If you are seeing behavior where dimensions and notes are shifting about wildly, then this is something that needs to be looked into with your reseller. In the meantime, you can use the above settings to see if they affect the results you see. System Options are system level settings, so it's a set once and forget. However, Document Properties need to be set in your Drawing Templates for future benefit, and within each existing (already created) drawing for benefit within that document.

I thought I could do something like recreate the problem but this is not going well. I have seen in in years past and it was usually after editing the part that some of the dims would go nuts, and balloons and notes attached to an edge would not be where they where supposed to be.